Exercise 1: Define Elements, Real Constants, Materials, Properties, and Components

In this step, you will load the ANSYS user profile in HyperMesh.

1. Start HyperWorks.
2. From the menu bar, click File > Solver Interface > Ansys.

In this step, you will retrieve and open the model file in HyperMesh.

1. From the menu bar, click File > Open > HyperMesh Model.
2. In the Open File dialog, select chapter2_1.hm.
3. Optional: If your model's elements and mesh lines are not shaded, click on the View Controls toolbar then select .

   
   
   Figure 1.

In this step, you will add an element type in HyperMesh.

1. In the Model Browser, right-click and select Create > Sensor from the context menu.
   HyperMesh creates and opens a sensor (Et Type) in the Entity Editor.

   
   
   Figure 2.

2. For Name, enter a new name for the Et Type.
3. Optional: For ID, enter a new ID for the Et Type.
   Note: By default, HyperMesh sets the ID to 1. If you create a new Et Type, HyperMesh will set the ID to n+1.
4. For Element Type, keep SHELL181.

   
   
   Figure 3.

   SHELL181

   Suitable for analyzing thin to moderately-thick shell structures. It is a 4-node element with six degrees of freedom at each node: translations in the x, y, and z direction; rotations about the x, y, and z axes (if the membrane option is used, the element has translational degrees of freedom only). The degenerate triangular option should only be used as filler elements in mesh generation.

   Well-suited for linear, large rotation, and/or large strain nonlinear applications. Change in shell thickness is accounted for nonlinear analysis. In the element domain, both full and reduced integration schemes are supported. SHELL181 accounts for follower (load stiffness) effects of distributed pressures.

   May be used for layered applications for modeling laminated composite shells or sandwich construction. The accuracy in modeling composite shells is governed by the first order shear deformation theory.

   Note: By default, HyperMesh set the Element Type to SHELL181. The elements in this model are of type SHELL181, therefore you do not need to change the element type for this tutorial.
5. Set the element stiffness (KeyOpt1), integration (KeyOpt3), layer data storage (KeyOpt8), thickness (KeyOpt9), and/or initial stress (KeyOpt10) options by selecting their corresponding checkboxes in the Value column as indicated in Figure 4.

   
   
   Figure 4.

   A value appears below each KeyOpt you selected.
6. For each KeyOpt you selected, keep the default value.
7. Optional: If necessary, from the menu bar, click View > Solver Browser to open the Solver Browser.
8. In the Solver Browser, review the ET Type you created.

   
   
   Figure 5.

In this step, you will define the properties of a material.

1. In the Model Browser, right-click and select Create > Material from the context menu.
   HyperMesh creates and opens a material in the Entity Editor.

   
   
   Figure 6.

2. For Name, enter Steel.
3. Optional: For ID, enter a new ID.
   Note: By default, HyperMesh sets the ID to 1. If you create a new material, HyperMesh will set the ID to n+1.
4. Click the Color icon, and select a color.
5. Set card image to MATERIAL.

   
   
   Figure 7.

6. Select the EX (Elastic moduli) checkbox.
7. For MP_EX_LEN (Number of Elastic moduli to input), enter 1.

   
   
   Figure 8.

8. For C, enter 2.1e5.

   
   
   Figure 9.

9. Select the NUXY (Minor Poisson's ratio) checkbox.
10. For MP_NUXY_LEN (Number of Minor Poisson's ratio to input), enter 1.
11. For C, enter 0.3.
12. In the MP_NUXY_LEN= dialog, enter 0.3.
13. Go to the Solver Browser and review the material you created.

In this step, you will create a section card for the model shell elements.

1. In the Model Browser, right-click and select Create > Property from the context menu.
   HyperMesh creates and opens a property in the Entity Editor.

   
   
   Figure 10.

2. For Name, enter SECTl.
3. Optional: For ID, enter a new ID.
   Note: By default, HyperMesh sets the ID to 1. If you create another new beam section collector, HyperMesh will set the ID to n+1.

   Ansys sections are supported under property, with a separate ID pool. Sections are created by setting the card image to SECTYPE. All cards created with the SECTYPE card image are organized under one ID pool. Properties created with a card image other than SECTYPE are organized under another ID pool. If you want to use the same IDs in these two pools, enable the allow duplicate IDs option from the menu bar by selecting File > Preferences > Meshing. In earlier versions of HyperMesh (14.0 or before), Ansys sections were supported under beam section collectors.
4. Click the Color icon and select a new color.
5. Set card image to SECTYPE.
6. For MAT, click Unspecified > Material.

   
   
   Figure 11.

7. Click the search icon.
8. In the Select Material dialog, select Steel.
9. Right-click on SECTION and select Create.
10. In the new Entity Editor, change the config to Shell, set the Tk value to 0.5, then click Previous.

    
    
    Figure 12.

11. For TYPE, click Unspecified > Sensor.
12. Click the search icon then assign sensor1.

    
    
    Figure 13.

13. In the Property folder of the Model Browser, right-click on SECT1 and select Duplicate from the context menu.
    HyperMesh creates a new property using the same card data as SECT1, except a different Name and ID are specified.
14. For Name, enter SECT2.
15. Click the Color icon and select a new color.
16. Leave MAT unchanged.
17. Go to the Solver Browser and review the two sections you created.

    
    
    Figure 14.

In this step, you will update each component with the respective element type, property, material, and section information.

1. In the Component folder of the Model Browser, click Base.
   The Entity Editor opens and displays the component's corresponding data.

   
   
   Figure 15.

2. For Property, click Unspecified > Property.
3. Click the search icon.
4. In the Select Property dialog, select SECT1.

   
   
   Figure 16.

5. In the Component folder of the Model Browser, click Rib.
   The Entity Editor opens and displays the component's corresponding data.
6. For Property, click Unspecified > Property.
7. In the Select Property dialog, select SECT2.
8. In the Component folder of the Model Browser, click mass.
   The Entity Editor opens and displays the component's corresponding data.

   Note: The mass component does not currently have a type, property, or material attached to it.
9. Create a property card that associates a small mass to the mass elements.
   1. Right-click on Property and select Create/Edit from the context menu.

      
      
      Figure 17.

   2. Set CardImage to MASS21p.
   3. Set KeyOpt3 to 3-D mass without rotary inertia.
   4. Under Real Constants, enter 0.001 for MASS.

      
      
      Figure 18.

   5. Click Close.

In this step, you will save the model to your working directory.

1. From the menu bar, click File > Save As > HyperMesh Model.
2. In the Save Model As dialog, navigate to your working directory and save the file.